BUG: Revolve Tool Broken in Latest Update

[jonwienke]

The latest update totally breaks the Revolve tool. I select a profile and can extrude it just fine, so I know my sketch geometry is good. When I select the same profile to Revolve, an edge of the profile as the rotation axis, and Revolve it, the preview shows correctly. But when I click OK, I get the following error message:

Error: Revolve1
<b>1 Reference Failures</b><br/>The profile reference is lost, try editing this the feature to reselect the lost profile.

The failed Revolve does not show up on the timeline, so I can't edit it to re-select the profile or rotation axis. It's completely broken and unusable now. I never had this problem with Revolve before the newest update.

[jhackney1972]

Please supply you model as well as a screencast showing your process.

[jonwienke]

Here's a link to a screencast showing the problem:
https://autode.sk/3hqU1k1

[jhackney1972]

I asked for your model also.  In the Screencast it would appear that you are trying to create a revolve body and "join" it to, what looks like a sketch.  This will give you an error.  If you changed your revolve to create a "new body" it will probably not fail.  I have tested the function this morning and see no issue.  If you continue to have issues, PLEASE attach your model for the forum users can troubleshoot it for you.

[jonwienke]

It's not just a sketch, it's a body set at 50% opacity. And I get the exact same error deleting all bodies and selecting "New Body":

https://autode.sk/3eJzZ2d

Note that this revolve is "Revolve2", implying that the Revolve1 I created previously still exists somewhere in the file, but isn't visible or accessible on the timeline.

[jhackney1972]

The two top sketch circle interfere with the revolve, change them to construction lines and all is well.  You can then use the sketch, lower down, to extrude the smaller hole.  I rearranged your body so it appears along with the sketch in the component.  The sketches seem to be not fully constrained either, I did not address that problem.  This is not a bug, just the creation of a confusing sketch for the modeler.  Model is attached.

[jonwienke]

Changing the circles to construction mode let me do the revolve. I didn't have to do that previously, and I had to incorporate the nozzle orifice into the revolve, rather than extrude the circle as I originally intended.

I appreciate the workaround, but still consider the issue to be a bug. The presence of a circle in the sketch that isn't part of the geometry selected for the revolve should have no effect on the revolve, and it shouldn't make the attempted revolve feature disappear from the timeline.

[TrippyLighting]

It might be a bug.

However, trying to design this as a single 3D sketch is utter nonsense!

[jonwienke]

It's definitely a bug related to revolving and extruding. I've had Fusion crash on me a couple times attempting to extrude a simple 2-point rectangle with a circle inside it, such that the extrusion has a hole in it. I submitted the automated bug reports already.

[TrippyLighting]

Don't use a 3D sketch for this!

[jeff_strater]

I agree - this is a bug.  Thanks, @jhackney1972 for the workaround.  No idea how you managed to find that, but that is good info for the dev team.  Also, I noticed this is a 3D sketch, though I don't understand if or how that might affect things.  Created bug FUS-69497 for this

I do not think this is a recent ("broken in the last update") change, I suspect that this is data-specific, and would have failed in previous versions, FWIW.  Profile recognition, Revolve, etc have not changed recently.

[jonwienke]

What's the point of 3D sketching capability if you can't use it? It's convenient to have all of the critical/mating surfaces for a part in a single sketch, rather than scattered among multiple sketches, especially when doing lofts and such.

[TrippyLighting]

I did not say that it does not have its use. I said not to use it in this case as it isn’t needed.
A general guideline for use of CAD tools is to use the simplest tool available to create a particular geometry.

It is a general noob mistake wanting to cram everything into one sketch. That approach, sooner or later is going to bite you.

One could argue that it already has 😉

[davebYYPCU]

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@jonwienke wrote:

.... in a single sketch, rather than scattered among multiple sketches, especially when doing lofts and .....

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Loft is already finicky, introduce 3d sketch to that tool, may bite harder....

Watching with interest....

[jonwienke]

Explain how using a loft is any different if the end profiles are in one sketch or different sketches. You're feeding it the same profiles either way.

[keqingsong]

This bug should be fixed in our latest January 2021 product update.